Don't Just Fill Your Oils ...

... Track Them ?

Why? I'm glad you asked !!

Did you know that filling your way lube tank can tell you a story about your machine's performance. It can, if you use the information to your advantage. How?

The best way is to make an oil fill reminder form and post it on the machine. Each time oil, any type of oil, is added to the machine, have the operator jot down the following:

• Type of oil added
• Date and Time the oil was added
• Amount of oil added
• On a turning center, when the chuck was greased

This data can be used for the following :

Type Of Oil : this tells you which oil tank might be giving you trouble. If you're filling the hydraulic tank (a closed system) - WHY and WHERE is the oil leaking from. Low hydraulic oil could result in a loss of pressure and perhaps an un-chucking of a part being machined with catastrophic results. If you're replacing way-lube (which you should), what kind of schedule are you on. This list should show a difference in the frequency of the filling which will easily and early show a way-lube system problem and head-off major repairs.

Date and Time the oil was added : this info gives you a clear view of the filling schedule. Again, not filling the way-lube tank, for example, will be easily seen and catastrophe can be averted.

Amount of oil added : as above, this info gives you a clear schedule of the filling schedule. Filling the way lube tank once every two days instead of once every three days will show up and might signal a line break or other problem that can easily be spotted and repaired in time.

As with everything in life, the info gathered is only as good as the person viewing it. Teach you operators to be hands-on people and to pay attention to this list, perhaps every morning with the machine start-up. Simple ideas like this TIP can help extend your machine's life and cut down dramatically on your machine's down time and repair bills.

Live Long ... and Make Chips !!

Spindle Load vs. Spindle RPM

Which is the true test of how hard your machine is working ?

If you had to watch the spindle speed meter or the spindle load meter on your CNC machine ... lathe or mill ... to determine if your machine was working too hard, which one would you choose?

The truth of the matter is that although the spindle load meter does tell you the power draw on the spindle motor, the RPM gage is a more accurate representation of how hard the spindle is working. Most machines come with a specific rating for load % per a specific time such as (in laymans terms) : "You can run this machine at 100% for 30 minutes."

That is of course a true statement and you can watch the load meter while cutting and reach that spec. However, if you watch the RPM gage while cutting and see it fluctuate wildly - basically because the motor is trying to keep the spindle at the specified (programmed) RPM - you'll never reach that 30 minute time frame. Because the cutting is so heavy in this type of case, the motor must keep "powering up" to keep the programmed RPM specified. This takes much more power draw on the motor than simply running constant at 100% load for the 30 minutes.

The Solution : When your machine is cutting, watch the RPM gage first to insure that the cutting conditions are resulting in a smooth RPM for the spindle and not wild fluctations as the motor fights to keep the speed constant. Secondly, adjust the cutting conditions so that the load meter is as high as you think you want (there is nothing wrong with 70-75%) and then recheck the RPM gauge to make sure that the RPM's are smooth at those settings. Smooth RPM cutting will result in better life for the spindle motor and smoother surface finish on the workpiece as well.

Happy Chip Making !!

Check out our Real World World machine shop software at www.KentechInc.com

Conversational CAD/CAM

Quoting & Estimating

G Code Conversion

CNC Training

.... and MORE !!!

Multi-Part Machining Series - Part #3

Machining Multiple - Different Parts

So far in our series we have looked at machining multiple parts of all the same part mounted in our fixtures during our machining cycle. What if we want to machine different parts during the cycle ... we want to mount different fixtures on the table and machine one of each during the machining cycle.

First let's look at some reasons WHY we might want to do this.

1. Perhaps we will be delivering an assembly made of multiple parts we need to machine. If we machine all the components at the same time ... during the machining cycle ... we can better accomplish scheduling and production of the entire assembly.
2. Perhaps similar parts utilize similar cutting tools ... if we can machine them at the same time we can reduce and better control our tooling requirements both from a "tool in the machine" as well as from an inventory viewpoint.
3. We need to break into a production run for some "special circumstance" ... rather than halt the production all-together, we can sneak another fixture on the table and machine both parts during the same cycle.
4. Having lived in the real world ... we could go on and on and on ... you know !!

Looking back at Part #1 and Part #2 in our series ... any of these scenarios certainly becomes a fairly simple task.

Fixture Offsets from Part #1
As we mount the different fixtures on the table ... we can establish a Work Offset for each fixture. Now each fixture is independent of the others ... and can be called with a simple G54-G59 call.


Sub-Programming from Part #2
We could use a variety of sub-programming options to accomplish the various scenarios. The easiest is to simply have a complete machining program for each fixture ... and call it using the sub-program call in our main program. So we would utilize a main program to actually link all our different machining programs together. Something line this :

Main Program :

O0001
G54
M98 P1234 ( program to machine fixture #1 completely )
G55
M98 P5678 ( program to machine fixture #2 completely )
G56
M98 P8888 ( program to machine fixture #3 completely )
M30
%


When we press the cycle start at program O0001 .... it will call each of our compete machining programs and will machine the workpieces at each fixture completely. Simple. You could get very creative and efficient if you did some specific tooling / sub-programming calls ... think about it.

And .... we still have our independent programs available should we need to just machine one of the parts for some reason.

As I'm writing this ... different scenarios and reasons to utilize this approach keep popping into my head. But rather than write a long dissertation here ... look around your shop ... look at your work flow ... and see if you can view some of your own scenarios where better work flow can be achieved using some of our talking points from this series.

If you are so inclined ... please drop us an email at Sales@KentechInc.com ... tell us some of your unique situations ... or even ask us our recommendations ... and we'll publish / add them into this post for the benefit of others to review.

Thanks in advance to everyone ... and Happy Chip Making !!

Check out our Real World World machine shop software at www.KentechInc.com

Conversational CAD/CAM

Quoting & Estimating

G Code Conversion

CNC Training

.... and MORE !!!

Multi-Part Machining Series - Part #2

Programming for Multiple Fixtures

So the decision has been made ... "We need production ... which means we need to mount as many vises or fixtures on the table as we can fit ... to make as many parts as possible."

First scenario ...

1. We are going to make all the same part. 
2. For our example here ... let's say that we can fit 4 fixtures on the table ... we are going to machine 4 parts in one cycle.

Some thoughts :

1. When the tool is in the spindle ... we want to do as much work with it as possible. That means hitting each part on each fixture while it's in the spindle.
2. As mentioned in Part #1 ... each fixture is independent with it's own work coordinate system.
3. As a set-up ... we want to make one part first ... confirm that it is correct dimensionally and that the cutting conditions are optimal ... and then expand those toolpaths to machine the other vises.
4. For this article ... we are not going to be concerned with the actual G code program ... more with the flow of the program. How we can structure the program to machine all the parts.

So we mount the fixtures on the table ... set up and record our Work Coordinate Offsets ... G54 - G57.

How can we write the program to machine one part ... then expand it to 3 more parts ... with the least amount of effort. Our suggestion : Sub Programming ( for a more in-depth MAKING CHIPS blog post on sub-programming ... go here : http://kipware.blogspot.com/2013/02/the-hows-and-whys-of-sub-programming.html )

Here is the structure of our initial set-up program :

O0001 ( Main Program )

N0001
G00G91G28Z0
T01M06
G90S3500M03
G43Z1.500H01M08 -------- Put the tool in the spindle, start the spindle, position Z to clearance

G00G54X0Y0 --------------- Move to the first fixture, call the sub to do the work with this tool
M98 P1000

G00G91G28Z0 --------------- End this tools sequence
M01

N0002
G00G91G28Z0
T02M06
G90S1200M03
G43Z1.500H02M08 -------- Put the next tool in the spindle, start the spindle, position Z to clearance

G00G54X0Y0 --------------- Move to the first fixture, call the sub to do the work with this tool
M98 P1001

G00G91G28Z0 --------------- End this tools sequence
M01

ETC
ETC -------------------------- Create similar cycles for all the remaining tools.
ETC
M30

Once all of the above is confirmed ... w're ready to rock and roll on all the fixtures.

Just make these simple edits :

O0001 ( Main Program )

N0001
G00G91G28Z0
T01M06
G90S3500M03
G43Z1.500H01M08

G00G54X0Y0
M98 P1000

G00G55X0Y0

M98 P1000

G00G56X0Y0
M98 P1000

G00G57X0Y0
M98 P1000

G00G91G28Z0
M01

N0002
G00G91G28Z0
T02M06
G90S1200M03
G43Z1.500H02M08

G00G54X0Y0
M98 P1001
G00G55X0Y0
M98 P1001

G00G56X0Y0
M98 P1001

G00G57X0Y0
M98 P1001

G00G91G28Z0
M01

ETC
ETC -------------------------- Create similar cycles for all the remaining tools.
ETC
M30

The above will work fine ... one blaring item is that we are positioning back to the first fixture ... from the last fixture each time ... some wasted movement. Easy to fix because of our structure and the use of sub-programs ... just start each tool at the last vise where the last tool was working ... like this :

First Tool :
G00G54X0Y0
M98 P1000

G00G55X0Y0

M98 P1000

G00G56X0Y0
M98 P1000

G00G57X0Y0
M98 P1000

Next Tool ( work the offsets backwards ):
G00G57X0Y0
M98 P1001

G00G56X0Y0

M98 P1001

G00G55X0Y0
M98 P1001

G00G54X0Y0
M98 P1001

Next Tool :

G00G54X0Y0
M98 P1002

G00G55X0Y0

M98 P1002

G00G56X0Y0
M98 P1002

G00G57X0Y0
M98 P1002

ETC ... ETC ... ETC.

So there you have it ... combining our knowledge of SUB-PROGRAMMING with WORK COORDINATE OFFSETS ... we machined (4) parts on (4) fixtures ... efficiently.

If you followed the other Making Chips posts on SUB-PROGRAMMING and WORK COORDINATE OFFSETS... you will have an even better understanding of why these features will prove so useful when :

1. Johnny "bumps" the middle fixture with his hammer
2. Paul adds a revision .... an additional hole to the part
3. "The Boss" decides he wants to take off one of the fixtures ... who knows why !!!

Anyway ... if you aren't sure why the above are simple fixes ... just go back and review the other posts !!

In the next post in the series ... we'll take a closer look at some other scenarios and options ... Stay Tuned !!

As always ... Happy Chip Making !!!

Check out our Real World World machine shop software at www.KentechInc.com

Conversational CAD/CAM

Quoting & Estimating

G Code Conversion

CNC Training

.... and MORE !!!

Multi-Part Machining Series - Part #1

Work Coordinate Systems

Most production shops will rarely utilize a one-vise or one-fixture setup on a VMC or HMC when running a multiple piece production run. The most efficient production will have the cutting tool performing it's function on as many parts as possible while it is in the spindle. That normally means adding as many multiple vises or fixtures as the room on the table will permit.

We will be devoting the next couple of Making Chips posts to set-up and programming tips and tricks dealing with multi-part machining.

What does that multi-part machining mean for programming? As with anything in life ... first we want to reduce the amount of work ... in this case, the amount of programming. The use of sub-programming to cut down on the amount of typing or data entry or whatever work ... is one. ( We dealt with sub programming in a previous post here : http://kipware.blogspot.com/2013/02/the-hows-and-whys-of-sub-programming.html ). The other is a little feature on most machines called WORK OFFSETS. In our post here we will be explaining the Fanuc style and codes of Work Offsets ... since about 95% of machines out there are what we refer to as "fanuc compatible." And that includes the popular Haas machines as well.

Why Work Offsets?

Let's take a simpler example of placing two vises on the VMC table ... both will hold identical pieces of stock ... and we want to machine two identical workpieces using the same identical tools.

Hole dimensions are identical for both workpieces.

We could always do something like use the top left corner on the part on the left as X0/Y0 and then add the 12.300 + 3.100 to program the two holes on the part on the right ... sure, simple in this case. But even this scenario is fraught with potential problems. 

1. What if we "bump" the vise ... and the 12.300 is no longer the case. We now have to go back into the program and adjust the X and Y coordinates to reflect the new distance. 
2. What if one vice is a different height / thickness than the other ... the parts Z0 is different.
3. Next time we run the job ... we have to get the vises exactly 12.300 apart ... or alter the program again.
4. .... it goes on and on ... none of the scenarios are nice to imagine.

This type of situation ... and this is a simple one ... begs for the use of Work Offsets.

What are Work Offsets?

The Work Offsets allow the user to designate distances from the fixed Zero Return position on the machine to a certain location on the machine through an offset table. The Work Offsets are recorded distances from a fixed position on the machine ... usually the Zero Return or Reference Return position on the machine. This position is the only position that can be repeated on the machine without fail ... because it is defined from a physical limit switch. Once the electronics on the machine are powered off ... most internally recorded positions are lost ... no power to keep the computer running, it loses it's memory. When the machine is powered back on ... we can find our Zero Return by utilizing that function on the machines panel because it searches for that physical limit switch ... it doesn't rely on any memorized position ... it is dependent on the physical limit switch. For that reason ... all Work Offset positions are recorded from that Zero Return position for all axis.

The number of Work Offsets available on a machine tool can vary ... some have as little as one or two and others have 300-500 ... on Fanuc controlled machines the standard number is six ... although options to add  more are available. They are designated by G code calls ... G54, G55, G56, G57. G58 and G59.

If you were to look in the Work Offset table ... you would see something similar to :

So the user measures the distance from the fixed Zero Return position to ... let's use our example ... to the top left corner of the left hand vice as that parts X0/Y0 location. The measured distance is then entered in the Work Offset table ... both X and Y ... under one of the Work Offset designations ... we'll use G54. The steps are repeated for the left hand vice ... and the X and Y distances are entered in the G55 offset locations.

In our example, let's imagine that the vises and the stock are the same height in the Z axis ... just for simplicity ... but the Z axis could have a value similar to X and Y if required.

How to use Work Offsets in the G Code Program?

Let's say we have the scenario below .... the machines Zero Return position is the point on the top right designated with the purple circle :

Our Work Offset Table would look like :

Now for the programming part. Whenever the G code calls out a Work Coordinate System .... G54 thru G59 ... that Work Coordinate System becomes the default and any X / Y / Z coordinates called out for in the G code will reflect the X/Y/Z coordinates from the offset table. So the programming line ...
G00 G90 G54 X0 Y0
 ... would move the tool to the top left corner of the left hand vise. If we were to then command ...
X3.100 Y-2.125
.... we would position to the top left hole of the left hand vise ... because the G54 Work Coordinate System is the default. Similarly ... the command lines :
G00 G90 G55 X0 Y0
X3.100 Y-2.125 
... would position the tool to first the top left corner of the right hand vise ... then the top left hole of the right hand vise using the G55 Work Coordinate System.

So using the Work Coordinate Offsets and Work Coordinate System calls ... it is very easy to switch between the left hand and right hand vise by simply commanding G54 or G55.

The Advantages of Work Offsets

As we outlined above ... we are asking for problems when we don't use the Work Offsets. How did we fix them?

1. If we "bump" the vise ... only the values in the Work Offset table will change ... the G code program will not need any editing.
2. If the vises were different heights .... we could easily use the Z value in the Offset Table to make that adjustment ... again, no program editing.
3. Next time we run the job ... we only need to adjust the G54 and G55 Offset Table values ... no program editing is required.
4. and on and on and on. I'm sure you will see many more advantages on the shop floor.

As we progress through our Multi-Part Machining Series over the next posts ... we'll try to highlight some of the other programming Tips and Tricks that can be employed.

Stay Tuned .... and Happy Chip Making !!

Check out our Real World World machine shop software at www.KentechInc.com

Conversational CAD/CAM

Quoting & Estimating

G Code Conversion

CNC Training

.... and MORE !!!

Your Way Lube System - Friend or Foe ?

Your CNC machine is equipped with an automatic oiler system. Great ! You won't have to think about oiling the machine and an alarm will tell you when the tank is dry. What a great device ? Right ?

Well, that is the design. Unfortunately, along with the "automatic" description of the system comes the "out of sight, out of mind" aspect of the system. Because many people know it is an automatic system, many people put it out of their minds and simply wait for the alarm to come up showing that the tank is empty and needs to be filled. But what if that alarm never comes on because the tank isn't empty ? Why wouldn't the tank be empty ?

As your machine gets older, the way lube system will require service just like any other mechanism. The main problem, which often gets overlooked, is that the "tank empty" alarm never comes on because the tank never drains and nobody ever notices it. Now your machine runs for months on end with no lubrication on the ways and when you finally notice a problem, it's too late. Here is the "Rest of the Story ..."

PROBLEM :  The machine's ways are not receiving any way lube oil.

SYMPTOMS - IN ORDER OF SEVERITY :

• Positioning / Repeatability Problems
• Axis makes noise when moving
• Axis Drive motor overload alarm coming when the axis is moving

POSSIBLE CAUSES :

• Way Lube Pump burned out.
• Way Lube Pump distribution flow set too low.
• Way Lube Pump filter CLOGGED
• Way Lube line BROKEN
• Metering Units are CLOGGED

POSSIBLE CAUSES EXPLAINED :

(1) Way Lube Pump Burned Out : If the way lube pump is burned out, obviously there will not be any lube getting into the system. These pumps are usually set using a timer system. There is basically two types of timer systems used :

• The pump is on a cam and the way it works is that the pump is always running. One gear turns another which acts like a step-down system and the second gear raises a "primer" lever. When the lever reaches the top of the stroke, the "primer" lever is released and the oil is pushed into the lines. This whole cycle can take 5-20 minutes meaning that even though the pump is always running, the lines get lube only every 5-20 minutes.
• How to Check It : Take a flashlight and look in the tank or remove the oil tank. Once looking inside, you can see the main gear that should be constantly moving. It may be at a very slow pace, but you will see it moving.

• The pump is set to an electrical timer set in the controls PC (programmable controller) or an actual physical electrical timer in the cabinet. This type of timer only supplies power to start the pump for every cycle.
• How to Check It : On some pumps there is no primer lever but a light comes on on the tank when the pump is activated. Make sure this light comes on every 5-20 minutes or some other sign comes on to show the pump is activated every 5-20 minutes.

(2) Way Lube Pump distribution flow set too low : As stated above, the way lube pump usually is set using a timer system. The flow amount that gets distributed into the lines during every cycle is usually set and adjusted at the pump with a manual setting mechanism. This type of adjusting mechanism is usually a knob that can be turned higher or lower to set more or less flow. Also, just look at the primer lever. During the mentioned 5-20 minute cycle, you should see the primer lever raise slowly and then start to drop after reaching the top of the cycle. Check the stroke of the lever - short stroke, less flow.

• How to Check It : The normal pump usage is in an 8 hour shift, you should fill the tank every 2-3 days. Also, you should see way lube flowing onto the ways. Always remember, the more flow the better. Yes, it may contaminate the coolant but that is better than ruining the ways and thus the machine just to save a couple of bucks.

The photo above shows a way lube pump unit which includes a manual flow control device. Adjusting the white knob adjusts the amount of lube being distributed per one cycle of the lube pump. When this type of pump is working correctly, you can see the white knob rising slowly then retracting, pushing the lube into the lines. The amount of rise and fall, and therefore the amount of lube distributed, is determined by the flow adjustment.

(3) Way Lube Pump filter CLOGGED : The way lube tank usually has a filter between the tank itself and the oil line that starts the distribution. This filter is usually in the tank itself at the bottom of the primer lever or in-line right after the main distribution line leaves the tank. It will get clogged over time, especially if there is no filter at the oil fill hole or if someone takes off the filter when filling the tank.

• How to Check It : Disconnect the main lube line where it exits the tank to feed the system or after the in-line filter if so equipped. When the cycle reaches the pump stage as outlined above, oil should flow through this connection. The flow should be strong at this point. If not, remove the oil tank and search out the filter or remove the in-line filter. They can often be cleaned with a cleaner but the best remedy is to replace it.

(4) Way Lube line BROKEN : Oftentimes a lube line in the system gets crimped or broken during machining or during service. These way lube systems are usually "pressurized" so to speak and if the pressure is released at one point, say at the broken line, the oil will flow all to that point, depriving all the other lines of fluid.

• How to Check It : When the pump is in the pumping stage, the primer lever should fall slowly. This is due to the fact that it is pushing the oil into the system. If a line is broken, the primer lever will fall quickly as all oil is funneled to the broken line area only. On systems without a primer lever, the pump may have a pressure gauge on the pump. During the pumping cycle, the pressure should register for a couple of seconds as the oil is pumped into the lines. If the pressure is low or does not come up at all during the pumping cycle, a line in the system may be broken.

(5) Metering Units are CLOGGED : In order to create the "pressure" of the system needed for even distribution, each oil line leads to a "metering unit" where the flow is lowered and the oil is discharged. When the pump forces oil into the lines, they all fill and flow to the metering units where the flow is stopped. Each metering unit is set to discharge the desired amount or "drops" of oil and perform their individual duties. Since some areas require more lube, the metering units can be different for each line or area. Since these metering units have actual valve type components in their very small bodies, over time these units can be become clogged or the inner workings can become stuck.

• How to Check It : This is a much harder area to check. The best remedy and prevention is to change these units every year as part of a yearly maintenance program. Because these units allow only drops to flow through, they are harder to see when troubleshooting. These metering units are usually located in "clumps" around the machine. Several lines lead to these central areas and lube lines are branched out from here to the various areas of the machine. Replacement metering valves should be obtained from the machine tool builder or dealer to insure that you are getting the correct replacement part. When changing these units, pay close attention to the flow arrow that is commonly marked on the units themselves. This arrow shows the direction of installation and flow. Check the original unit before removal and replace accordingly.

The photo above shows an example of some metering units. These individual fittings are usually located in one or two main terminal blocks that feed certain areas of the machine such as the axis and ball screws. As the system fills with pressure and lube, these fittings discharge the lube at their pre-set flow rate into their lube lines. Over time, like cholesterol in the arteries, these units become clogged and no longer allow lube to exit and thus deny vital areas of the machine the way lube they require. As part of a yearly maintenance program, metering units in the machine should be replaced as a precautionary measure.

Due diligence and a little tracking will 

insure your Happy ( and ACCURATE ) Chip Making

 for years to come !!

Check out our Real World World machine shop software at www.KentechInc.com

Conversational CAD/CAM

Quoting & Estimating

G Code Conversion

CNC Training

.... and MORE !!!

Canned Cycle Drilling and R Plane Tricks

Wasting time drilling air when "drilling" holes in a part with multiple levels is not uncommon for the novice programmer. In this Making Chips post ... we would like to discuss the always important R plane and how you can easily control it in your G code program.

First ... the FACTS :

There are two planes that the programmer needs to be concerned with :

INITIAL PLANE ... this is the plane used for rapiding around the workpiece. This plane should always be set high enough to avoid the workpiece as well as any clamps or other fixture related objects that can be struck by the tool as it moves around the part.

• On  Fanuc controlled or Haas machine ... the initial plane is defined as the last Z position before the canned cycle is called. So in the sample code below :

G00 G90 Z1.000

G98 G81 Z-.500 R.050 F1.0

• Z1.00 would be considered the INITIAL PLANE ... because it is the last Z position prior to the the G81 canned cycle command.
• In an Okuma machine ... the user can set the INITIAL PLANE by commanding a G71 Z--- line prior to the canned cycle command line. So ... imitating the above Fanuc line ... we would program :

G71 Z1.000

G81 Z-.500 R.050 F1.0

R PLANE : The R plane is defined as the plane at which the drilling operation begins. So basically the tool rapids from the Initial Plane to the R plane ... and then starts the drilling operation. The R plane is defined in the canned cycle command line. So in the above examples ... R.050 is defined as the R plane ... the point where the drilling operation would begin.

In the above programs ... the tool would rapid from the Z1.00 initial plane to the Z.050 R plane.

After drilling ... we can tell the tool where to return by using the G98 ( initial plane return ) or G99 ( R plane return ) ... for Fanuc / Haas ... in the canned cycle command line. Once commanded ... G98 / G99 becomes modal ... which means the machine will remember where it is supposed to return ... until told differently. When programming for Okuma ... we can use the M53 ( like G98 ) / M54  ( like G99 ) commands.

NEXT ... the TRICKS :

Did you know that you can very easily change the R plane when drilling on uneven surfaces?

Did you know that you can very easily change the return point between the INITIAL and R planes?

As mentioned above ... once G98 or G99 is set ... the control remembers where to go.

Also ... once the R plane is set in the canned cycle command ... it remembers where the R plane is.

But you can change either very easy ... just command it !! Like this :

(1) G00 G90 Z1.000

(2) G98 G81 Z-.500 R.050 F1.0

(3) X1.00 Y1.00

(4) G99 X2.00 Y2.00

(5) X3.00 Y3.00 R-.100

(6) G98 X4.00 Y4.00 R.050

(7) G80

(1) - Sets the Initial Plane as Z1.00

(2) - Sets the R plane as Z.050 ... return to the Z1.00 after drilling this hole

(3) - Drill this hole ... R plane is .050 and return to Z1.00 ... these were modal from (2)

(4) - After drilling this hole ... return to R plane ... still set to Z.050

(5) - Drill this hole but start at the new R plane of Z-.100 ... return to Z-.100 after drilling ... G99 is modal.

(6) - Drill this hole but start at the new R plane of Z.050 ... return to Z1.00 after drilling this hole G99.

(7) - Cancel the canned cycle ... all modal canned cycle information is cleared.

On an Okuma machine ... users can set and re-set the Initial Plane through the G71 command. On a Fanuc / Haas control ... this is not so easy. You would have to cancel the current canned cycle with a G80 ... move the Z axis to the desired Initial Plane ... then re-command a new canned cycle to set a new Initial Plane.

So ... as we illustrated here ... it's fairly easy to efficiently and effectively machine holes on uneven surfaces using a combination of the return plane commands G98 / G99 / M53 / M54 and R plane settings. Although the Initial Plane. So ... STOP CUTTING AIR !!!

Happy Chip Making !!

Check out our Real World World machine shop software at www.KentechInc.com
Conversational CAD/CAM
Quoting & Estimating
G Code Conversion
CNC Training
.... and MORE !!!

G28 - Do you REALLY Know What It Does?

Most programmers use the FANUC G28 command to return an axis to the ZERO RETURN or REFERENCE RETURN position for a variety of reasons. Because this position is normally the position of the axis almost at one end of the stroke, those reasons range from tool change considerations to clearance considerations to safety considerations.

On a CNC lathe, REFERENCE RETURN or ZERO RETURN is the normally the axis at the farthest position away from the chuck - used mostly for safety and clearance reasons. On a vertical machining center, the Z axis is normally required to be at this position for a tool change sequence to start - an alignment issue here.. On a horizontal machining center, both Z and Y may be required to be there for a tool change alignment.

The How's & Why's of ZERO RETURN ?

The ZERO RETURN position is a very important position to the machine tool because this position never changes, even after POWER OFF. Basically, the ZERO RETURN position is a fixed position in which the machine tool builder uses a physical limit switch to obtain. The normal mode of operation when finding ZERO RETURN is that the axis rapids in the zero return direction looking for the signal from the limit switch that the dog has made contact. At that point, the axis slows to a feedrate set within the control and feeds until the dog feeds off the switch. At this point, the axis will begin to feed at a slower rate, a set number of pulses of the motor or set number of turns of the ballscrew. This final distance is called the GRID SHIFT and is usually adjustable through the machine parameters.

This type of system assures that the ZERO RETURN position will be arrived at even after power off and will be the same position, within tenths, all the time. For this reason, the ZERO RETURN position is very important to the machine tool and the programmer. It is the only position on the machine that can be found again and again after power off - because of the use of the "hard wired" limit switch. For this reason, most work coordinate systems (G54-G59) and PART ZERO locations are measured from the ZERO RETURN position.

In the newer machines and newer controls (referencing FANUC controlled machines with "red cap" axis drive motors), the zero return position is memorized within the control. Although the "hard wired" limit switch is used to set the position initially and after a CNC failure, once the position is found it is memorized in the control. This allows for a much faster movement to ZERO RETURN either through the program or in the manual mode. This system is commonly referred to as DOGLESS ZERO RETURN.

Usually on older machines, after POWER OFF, it becomes necessary to re-establish the ZERO RETURN position before operation can begin. Therefore, the first act upon power on of the machine should be to return the machine to the ZERO RETURN either by the manual method or thru the programmed G28 command. Oftentimes, machines are set up and will not allow automatic operation until manual reference point return is completed. This type of machine set up restricts the initial reference point return to manual operation only.

The Program and Zero Return ?

As mentioned above, it often becomes necessary in a program to send one or all of the axis to the ZERO RETURN position for any of the reasons outlined above. This can be accomplished in the program through the G28 - Return to Reference Point command. Although most programmers use this command, I have encountered many instances when I ask them why and how they use it, they simply say, "I don't know, that's the way we do it and it works?"

Like all movement commands, G28 can be made in either the ABSOLUTE mode (G90) or INCREMENTAL mode (G91). In either case, the movement is always made through an INTERMEDIATE POINT in the G28 command. The intermediate point is a point the tool will go through before proceeding to the ZERO RETURN position.

If G28 is commanded in the ABSOLUTE mode, that is with an absolute dimension after the G28, this absolute dimension is regarded as the INTERMEDIATE POINT and the machine tool will first go to this point before moving to reference return. For example, used in a machining center, one might command :

Machining Center Ref. : G00 G90 G28 X4.00 Y2.00 ;

Lathe Ref. : G00 G28 X4.00 Z2.00 ;

The above command would move the tool from the current position to the absolute position of X4.00 and Y2.00, then to the X and Y axis reference point return position. This is movement through an absolute INTERMEDIATE POINT. This can be used for safety or clearance reasons and eliminates the need for a seperate move to the clearance point than another command to the zero return position.

When used in the INCREMENTAL mode, the G28 can produce a move directly to the zero return position. For example, the machining center command of :

Machining Center Ref. :G00 G91 G28 X0 Y0 ;

Lathe Ref. : G00 G28 U0 W0 ;

The above command actually establishes an intermediate point of with an incremental distance in X and Y of 0. Therefore the tool moves to the intermediate point (no movement) then to the reference point. The end result is a direct move to the reference point. This is commonly used in programming.

As stated in the above examples, the Return to Reference Point is performed using the modal G movement command (G00 or G01) if not commanded in the same line as the G28 command. Therefore, good programming practice is to include the G00 or G01 on the same line as the G28 command.

Happy Chip Making !!

Check out our Real World World machine shop software at www.KentechInc.com

Conversational CAD/CAM

Quoting & Estimating

G Code Conversion

CNC Training

.... and MORE !!!

The How's and Why's of Sub Programming

If you have done any manual G code program creation, you know you are always looking for some shortcuts  that can not only help cut down the data input ... but would also help eliminate errors. Whether they be typing errors or movement errors ... the less chance to create one the better.

One of the more powerful tools available to a programmer is the use of SUB PROGRAMMING. In this Making Chips post ... we would like to touch on some of the basic ideas, concepts and uses for sub programming. This post will illustrate the Fanuc / Haas coding format ... but check out the end of the post for Okuma explanations as well.

What is a Sub Program?
Basically, a sub program is a G code program that is called from another G code program. The contents of the sub program is not limited and can contain tool calls, spindle calls ... just about anything any other G code program can contain. The sub program itself resides in memory under it's own program number ... and is separate from the "main program".

Why Would I Use a Sub Program?
As mentioned above ... the less data entry means less chance for a mistake. let's take this example scenario where we have to let's say spot drilling then drill then chamfer then tap a series of holes. The less times we have to re-type those hole locations, the less chance we will have a typo and / or put a hole in the wrong place. If we can store the X / Y coordinates of the hole locations in one location and call them out as needed ... that saves data input and reduces our chances for errors. This is a good example of how a sub program ( in this case it would be the program that stores the hole locations ) can be a big help.

How Do I Program and Call a Sub Program?
A sub program scenario consists of a main program and the sub program. The main program consists of all the code that doesn't repeat itself ... the sub program consists of all the data that will be repeated. In our above example ... the tool calls, spindle calls, drilling cycles will all be different for each hole ... so we will store that in the main program ... but the hole locations will be the same so we will store them in the sub program.

When you create a sub program ... it is done just like you would create any other program. On Fanuc / Hass controls you start out with an O number ... and type the program as normal. Let's take our above example of hole locations ... the sub program might look like this :

O1234
X1.1 Y1.1
X2.2 Y2.2
X3.3 Y3.3
X4.4 Y5.5
M99
%

Notice that we have an M99 at the end ... not an M30 or M02 like a normal program. This indicates that this is a sub program ... we'll explain the M99 command a little later.

This program is entered in the control as any other program ... and resides in it's own memory space.

When a Fanuc / Haas control wants to call a sub program to run ... the programmer issues an M98 command in the Main Program. The M98 command is also followed by a P address ... which is the "O" number of the external program to run. Our above sample sub program would be called with the command :
M98 P1234

When the main program reads the M98 command ... it jumps out of the main program and starts to execute the sub program ... in this case program O1234.

When it reads the M99 command at the end of the sub program ... it jumps back to the main program to the line after the one through which it left. In other words, it jumps back to the line after the M98 command.

The Complete Story
Let's take a look at the full program and the sub program calls ... see if you can follow the path.

Main Program
O0001
G00G91G28Z0
G28X0Y0
M01
N0001
(SPOT DRILL)
G00G91G28Z0
T01M06
G90S3500M03
G00X1.100Y1.100
G43Z.500H01M08
G99G81Z-.130R.050F20.0L0
M98P1234
G80
G00G91G28Z0
M01
N0002
(DRILL)
G00G91G28Z0
T02M06
G90S3000M03
G00X1.100Y1.100
G43Z.500H02M08
G99G73Z-875R.050Q.125F20.0L0
M98P1234
G80
G00G91G28Z0
M01

ETC.    ETC.    ETC.

M30
%

Sub Program
O1234
X1.1 Y1.1
X2.2 Y2.2
X3.3 Y3.3
X4.4 Y5.5
M99
%

Can you follow the path as the program jumps to the sub program?

Here is an in-depth explanation.

N0001 
(SPOT DRILL)
G00G91G28Z0
T01M06
G90S3500M03
G00X1.100Y1.100 --------------------- Position to our first hole.
G43Z.500H01M08 --------------------- Bring the Z axis to the clearance plane.
G99G81Z-.130R.050F20.0L0 ---------- Call our canned cycle ... but use L0 which means 
                                                                the control will hold the data ... but will not
                                                                execute the cycle.
M98P1234 ----------------------------- Jump to our sub program O1234 which will cause a
                                                                hole to be spotted at each X / Y location in the sub.
G80 -------------------------------------When the M99 is read ... the program will jump 
                                                                back to here.
G00G91G28Z0
M01


N0002 ---------------------------------- This sequence basically does the same thing ...
                                                                except we are establishing a different
                                                                canned cycle before we jump to the sub program.
(DRILL)
G00G91G28Z0
T02M06
G90S3000M03
G00X.100Y.100
G43Z.500H02M08
G99G73Z-875R.050Q.125F20.0L0
M98P1234
G80
G00G91G28Z0
M01

Another Example ...
Once you are able to follow the above ... here is another scenario.

You can also call a sub program and have it executed a set number of times. Let's take the example where we want to execute a program on our lathe to make a washer (3) times. We will enter the main program and sub program as below.

Main Program :
O0001
M98 P1234 L3
M30
%

Sub Program :
O1234
*********
between here is the complete machining program that includes
tool calls ... spindle calls
the feeding of the stock
the machining of the part
the cut-off of the part
*********
M99
%

The cycle start is executed with program O0001 ... which calls the sub program O1234 and executes that program (3) times ... the L in the M98 line. This feature is different for the various Fanuc controls but is usually commanded either :

M98 P ---- L
or
M98 P****$$$$ where **** is the program number and $$$$ is the number of times to repeat.

Differences Between Fanuc / Haas and Okuma OSP
The basic ideas of calling and executing a sub program is the same between these controls ... the G code commands are a bit different. Those differences are outlined below.

Sub Program Call
Fanuc / Haas : M98
Okuma : CALL
Example : CALL O1234 will call sub program O1234

Sub Program End
Fanuc / Haas : M99
Okuma : RTS

Sub Program Call with Repeat
Fanuc / Haas : M98 P1234 L5 or M98 P12345
Okuma : CALL O1234 Q5 with the Q value being the number of repeats.

That's basically it ... just some G code differences but the basic idea and execution is the same.

**************************************

Sub programming is a powerful tool ... even if you are not trying to avoid re-typing and repeated data entry. Hopefully this Making Chips post will get you thinking and exploring all the ways sub programs can make you a better programmer.

Happy Chip Making !!

Check out our Real World World machine shop software at www.KentechInc.com

Conversational CAD/CAM

Quoting & Estimating

G Code Conversion

CNC Training

.... and MORE !!!

Move That Vise !!

MOVE THAT VISE !!! ... It could mean more years for your machine tool.

It seems the simpler, often overlooked things can be the downfall of most shop equipment. Focusing on a few simple ideas can avoid those big repair bills and keep machine tools running like new much longer.

When most setups are done on a VMC, the workholding fixture is neatly mounted right in the middle of the table. Although it looks good, this is actually one of the worst "habits" for the machine. Locating the vise or fixture in the same place has the following harmful effects on the life of the machine:

• Table wear, resulting in dip or sag in one spot.
• Boxway or guideway wear on or around the spot, causing loose surface and gib contact, and shuck in the ways.
• Ball screw wear, resulting in excessive backlash in that one area of the screw, which cannot be repaired through CNC compensation.

Of course you're going to clean the 

table completely before installing the vise.

Then are you going to place the vise so

it looks nice and neat in the center of the table?

NO !!!

Placing the vise or fixture in or around the same area of the machine table will cause all of the above, with the most common symptom over time being backlash of the screw. When trying to compensate and set the backlash, the person making the repair will often find different backlash values when checking along the length of the axis stroke. This most often results in the need to replace the whole ball screw. Because most CNC machine controls only permit one backlash compensation value to be set in the parameters, compensating for the backlash cannot be effectively performed through the control.

You also may find that the gibs need to be adjusted in that area of the boxway, because the axis has some side-toside movement to it when moving. Squareness in that area will disintegrate; and, in the worst case, this shucking can be heard when the axis changes direction. The most common remedy of adjusting the gib in that area causes the axis to bind when it reveals to the other areas, because the boxway wear is different along the stroke. In this repair, the machine's boxways may need to be reground, rescraped or both. In either of these cases, the repair bill will be huge.

The remedy is to make sure to move the vise or fixture location around on the tabletop whenever possible. You will see a more consistent wear pattern for the machine, and any backlash that occurs can be taken up correctly through the control. You will not be able to stop machine wear, but you can distribute it more evenly along the machine, which provides a longer life for all the components involved.

Happy Chip Making !!

Check out our Real World World machine shop software at www.KentechInc.com

Conversational CAD/CAM

Quoting & Estimating

G Code Conversion

CNC Training

.... and MORE !!!

Roughing Canned Cycle in Turning - Part 2

This post is continuing with the important feature of programming canned cycles for rough turning. In Part 1 we discussed the general outline, format and command lines for the cycles ... in Part 2 we want to illustrate some examples using Fanuc ( and therefore Haas ) programming that hopefully we give an even clearer picture of the uses and commands for these cycles. We do have some Okuma Programming Notes at the bottom of this post.

The examples will use the same shape ... but will illustrate the to main Fanuc cycles for bar stock roughing ... G71 -Turning and G72 - Facing.

G71 will produce a cutting motion along the Z axis ... generally referred to as a turning motion. The G72 cycle will produce a cutting motion along the X axis ... or a facing type motion.

The way we position our Points A - B - C will also determine the motion as illustrated below. The general rule of thumb is to describe the cutting motion through the finish contour code in a motion that moves from A to B along the contour to C. This description will assist you in placing Points A - B - C in their correct location in relation to the part and the contour.

___________________________________________________________

Example #1 : 
OD Cutting Along the Z axis - Turning

(1) First we established our points A - B - C and using a clearance amount of .100 in X and .050 in Z.

(2) In our program ... the first step is to rapid to point A ... N1000 = our P call in the canned cycle block.

(3) Then command the Canned Cycle Call

(4) Then rapid to point B and proceed around the part contour to point C ... N1100 = our Q call in the canned cycle block.

G96S650M03

G00X11.0Z1.0M08

G00X10.3408Z0.05

G71P1000Q1100U0.01W0.01D0.1F0.012

N1000G00X4.8729.0Z0.05

G01X4.8729.0Z0.0F0.012

G01X4.8729Z-1.2967F0.012

G01X6.9769Z-1.998F0.012

G01X6.9769Z-3.4277F0.012

G01X10.2409Z-3.4277F0.012

N1100G00X10.3408Z-3.4277

G00X10.3408Z0.05

___________________________________________________________

Example #2 :
OD Cutting Along the X Axis - Facing

By re-arranging Points A - B - C ... and using the G72 cycle ... we can change the cutting direction from turning to facing. The basics of the format and steps in the program are the same ... move from A to B along the contour to C ... and this will help us position Points A - B - C.

G96S650M03

G00X10.1000Z1.0M08

G00X10.3408Z0.05

G72P2000Q2100U0.01W0.01D0.1F0.012

N2000G00X10.3408Z-3.4277

G01X10.2408Z-3.4277F0.012

G01X6.9769Z-3.4277F0.012

G01X6.9769Z-1.998F0.012

G01X4.8729Z-1.2967F0.012

G01X4.8729Z0.0F0.012

N2100G00X4.8729Z0.05

G00X10.34Z0.05

___________________________________________________________

Example #3 :
ID Rough Cutting Along the Z Axis Turning

Now let's turn things to focus on ID cutting. Again ... the same procedures and rules apply ... flip Points A - B - C to reflect cutting the ID rather than the OD. The same rule applies ... move from A to B along the contour to C.

G96S650M03

G00X.9717Z1.0M08

G00X0.9717Z0.05

G71P1000Q1100U-0.01W0.01D0.05F0.012

N1000G00X2.7117Z0.05

G01X2.7117Z0.0F0.012

G01X2.7117Z-0.8633F0.012

G01X1.7622Z-1.6563F0.012

G01X1.0717Z-1.6563F0.012

N1100G00X0.9717Z-1.6563

G00X0.9717Z0.05

___________________________________________________________

Example #4 :
ID Rough Cutting Along the X Axis - Facing

And again ... by re-positioning Points A - B - C and using G72 ... we can perform the rough cutting using cutting from the centerline out in a facing motion.

G96S650M03

G00X1.0Z1.0M08

G00X0.9617Z0.05

G72P2000Q2100U-0.01W0.01D0.05F0.012

N2000G00X0.9617Z-1.6563

G01X1.0717Z-1.6563F0.012

G01X1.7622Z-1.6563F0.012

G01X2.7117Z-0.8633F0.012

G01X2.7117Z0.0F0.012

N2100G00X2.7117Z0.05

G00X0.9617Z0.05

___________________________________________________________

Okuma Programming Notes :

Okuma OSP controls refer to the cycles as illustrated above as LAP cycles. The format and use is pretty basically the same as described for Fanuc / Haas controls with some modifications. If you can understand the outlines above ... the notes below should get you through the differences between the Fanuc / Haas format and that required by OSP controls.

1. For motion for both turning and facing ... command a G85 as the canned cycle command. The variables in the G85 line are outlined in Part 1 of this series.
2. On the line immediately following the G85 call ... command a G81 for turning or G82 for facing. This G code should appear on a line by itself with no other code on the line.
3. The N number command on the G85 line should refer to the N number of the line where the G81 / G82 is commanded.
4. At the end of the sequence that describes the finish contour ... command a G80 on a line by itself to signify the end of the finish profile sequence.

The Fanuc / Haas code from example #1 above has been transposed for the Okuma OSP format below :

G96S650M03

G00X11.0Z1.0M08

G00X10.3408Z0.05

G85 N1000 U0.01 W0.01 D0.1 F0.012

N1000 G81

G00X4.8729.0Z0.05

G01X4.8729.0Z0.0F0.012

G01X4.8729Z-1.2967F0.012

G01X6.9769Z-1.998F0.012

G01X6.9769Z-3.4277F0.012

G01X10.2409Z-3.4277F0.012

G00X10.3408Z-3.4277

G80

G00X10.3408Z0.05

___________________________________________________________

They say a picture is worth a thousand words ... hopefully the illustrations here will help you solidify your programming of these powerful and important canned cycles.

If anyone notices any errors in this post ... please leave a Comment below and straighten it out ... to benefit anyone stopping by ... and Thanks in advance.

Happy Chip Making in 2013 !!

Check out our Real World World machine shop software at www.KentechInc.com

Conversational CAD/CAM

Quoting & Estimating

G Code Conversion

CNC Training

.... and MORE !!!

Roughing Canned Cycle in Turning - Everything You Need to Know - Part 1

Canned cycles in CNC controls are powerful features that when used correctly can reduce programming commands and increase program efficiency dramatically. There are a variety of cycles available on most controls, the most powerful are stock removal or roughing cycles. In most of these type of cycles, the user can define the roughing process and cutting parameters, then simply describe the finish shape using G codes. The control will then auto-calculate start and end points as it removes the material to leave the workpiece with the finish shape profile.


Let's start out by explaining WHY THIS IS IMPORTANT !!!

1. No depth of cut or point calculations required ... all you need to do it describe the finish profile and the control does all the work.
2. Cutting conditions in the real world are dictated by the actual process of stock removal. Sure you're sitting in your office and writing the program ... everything looks great ...  inevitably when you start to actually do the cutting, things change. When using a canned cycle ... to change the depth of cut ... finish allowance ... feedrate ... they are all just edits to one variable in the canned cycle line. What could be easier !!! If you wrote the code long hand ... you have to re-generate the code each time you want to make any of these changes.
3. ENUF said ... the CORRECT way to program any rough cutting is to use a canned cycle ... period. Whether through a CAD/CAM system or whatever. Anybody who tells you different is a poor programmer.

The cycle will will outline in this blog post is the G71 cycle in Fanuc / Haas controls ... and the G85/G81 cycle in Okuma OSP controls. This cycle will remove the material along the Z axis, taking depth of cut along the X axis. The command line will define the cutting parameters such as depth of cut, feedrate and finish material to leave as well as telling the control where to look for the finish profile of the part. Usually the command line includes (2) N numbers or some other start / end variables. The control looks between these start / end variables to see what the finished shape looks like. The user uses what amount to a standard finish cut G code program to define that finished shape and places that G code in-between those start / end variables.

For the CNC controls covered here, the same basic programming format  and programming steps should be observed. The first steps are to establish three points that are required to help describe to the CNC control the finished shape desired. These are outlined in more detail in the ANIMATION sequence for this code.

A) Pt. A : Clearance point in the X axis
 Clearance point in the Z axis

B)  Pt. B : Along the X plane established by Pt. A, last X diameter of the profile
 Same Z axis plane as Pt. A.

C) Pt. C : Same X plane as Pt. A.
 Along the Z plane as established by Pt. A, last Z face along the contour.

Once the three points above are calculated, the following programming sequence can be used :

a) Start the tools process as normal which means index the tool and start the spindle.

b) Rapid the tool to point A using the normal format rapid approach.

c) Command the CANNED CYCLE block as explained below.


FADAL, HAAS & Fanuc Controls ( Models 6,10,11,12,15 ) :
G71 Pxxxx Qxxxx Uxxxx Wxxxx Dxxxx Fxxxx ;
P = Sequence (N) number of the first block of the finish shape program.
Q = Sequence (N) number of the last block of the finish shape program.
U = Amount and direction of the finish allowance in the X axis ( diameter value in diameter
programming ).
W = Amount and direction of the finish allowance in the Z axis.
D = Depth of cut (radius value) - no decimal point allowed (format = xxx.xxxx) - no sign allowed.
F = Feedrate in roughing - this value overrides any feedrate commanded between P and Q.

Option : S and T commands - Good programming practice would place these commands active earlier in the programming sequence.

Fanuc Controls :
( Models 0,16,18,20,21 )
G71 Uxxxx Rxxxx ;
G71 Pxxxx Qxxxx Uxxxx Wxxxx Fxxxx ;
U = Depth of cut - radius value
R = Retract Amount - the amount the tool will retract before returning to the start for next depth
of cut.
P = Sequence (N) number of the first block of the finish shape program.
Q = Sequence (N) number of the last block of the finish shape program.
U = Amount and direction of the finish allowance in the X axis ( diameter value in diameter
programming ).
W = Amount and direction of the finish allowance in the Z axis.
F = Feedrate in roughing - this value overrides any feedrate commanded between P and Q.

Option : S and T commands - Good programming practice would place these commands active earlier in the programming sequence.

OSP Controls :
G85 Nxxxx Dxxxx Fxxxx Uxxxx Wxxxx ;
N = Sequence (N) number of the first block of the finish shape program. Last sequence is described as the line containing the G80 command.
D = Depth of cut (radius value).
F = Feedrate in roughing - this value overrides any feedrate commanded between P and Q.
U = Amount and direction of the finish allowance in the X axis ( diameter value in diameter
programming ).
W = Amount and direction of the finish allowance in the Z axis.

Option : S and T commands - Good programming practice would place these commands active earlier in the programming sequence.

d) Continue the program by programming the finish shape starting with a rapid move from Pt. A to Pt. B.. The type of command used here (G00 or G01) will determine the roughing cycle move as it moves in this direction during the roughing process. This block must be labeled with the start sequence number specified in the call in the CANNED CYCLE block.

Fanuc control's have two types of canned cycles called TYPE I and TYPE II. The TYPE I cycle only allows for finished shapes where the axis are moving in one direction ... which basically means that no type of "pockets" can be included in the contour. TYPE II cycles are generally an option but do allow for non-continuous type contours.

Initiating a TYPE I or TYPE II cycle takes place in this block ... the move from POINT A to POINT B. If a two axis move ... both X and Z or U and W are included in this block ... than a TYPE II cycle is initiated if available. If the option is not present ... an alarm is usually generated alerting the user that the option is not available.

In the above example ... and since the Z axis plane of Point A and Point B should be the same ... an incremental move of zero in the axis is usually included just to get the cycle initiated. For example :
G00X1.250W0;
... this move will not effect the movement but since both an X and Z move are commanded ... the TYPE II cycle will be initiated.

e) Complete the program for the tool path to go all around the part contour from Pt. B around the part and ending at Pt. C. You may use G01, G02 or G03 for tool movement as long as the shape is always vertical in the X axis and horizontal in the Z axis. No pocketing is allowed in the shape (Type I only - Type II canned cycles do have this capability). This block must be labeled with the end sequence number specified in the call in the CANNED CYCLE block.

f) Finish the program with a rapid move from Pt. C back to Pt. A. The type of command used here (G00 or G01) will determine the roughing cycle move as it moves in this direction (retract) during the roughing process.

g) Return the tool, like normal, to the indexing position or, while the tool is at Pt. A, call the FINISHING CANNED CYCLE using the same P and Q sequence numbers to finish the part with the same tool.

This outline is fairly complete ... but it may take a little trying and testing for you to get the hang of it ... but the benefits are worth the effort. The ease of editing the cutting conditions and changing or altering the profile make this cycle powerful and real world. If you can master the use of this cycle ... you will reap the benefits for the rest of your programming life. If someone tells you different ... don't believe them.  And if you run across someone who never uses it or doesn't know how to use it ... consider them a poor programmer.

Happy Chip Making !!

Check out our Real World World machine shop software at www.KentechInc.com

Conversational CAD/CAM

Quoting & Estimating

G Code Conversion

CNC Training

.... and MORE !!!